How to 'probe' principal stresses for a set of nodes?

Not really a probe, but I suggest the following which will display a message box with the values of the principal stresses. It uses DPF.

import math
import units
import mech_dpf
import Ans.DataProcessing as dpf
 
clr.AddReference("Ans.UI.Toolkit.Base")
clr.AddReference("Ans.UI.Toolkit")
from Ansys.UI.Toolkit import *
 
curSel=ExtAPI.SelectionManager.CurrentSelection
 
# Need to have two faces selected, otherwise pass
if (curSel.Ids.Count==0):
    mess_line1 = 'Please select at least one node'
    MessageBox.Show(mess_line1)
    pass
 
meshData=ExtAPI.DataModel.Project.Model.Analyses[0].MeshData
 
scoping=dpf.data.Scoping()
scoping.Ids = curSel.Ids
scoping.Location=dpf.enums.location.nodal
 
 
an1=ExtAPI.DataModel.AnalysisByName(ExtAPI.DataModel.AnalysisNames[0])
rstFile=an1.WorkingDir+'file.rst'
 
dataSource = dpf.data.DataSources(rstFile)
 
stressOp1 = dpf.operators.result.stress_principal_1()
stressOp2 = dpf.operators.result.stress_principal_2()
stressOp3 = dpf.operators.result.stress_principal_3()
 
stressOp1.inputs.data_sources.Connect(dataSource)
stressOp2.inputs.data_sources.Connect(dataSource)
stressOp3.inputs.data_sources.Connect(dataSource)
 
stressOp1.inputs.mesh_scoping.Connect(scoping)
stressOp2.inputs.mesh_scoping.Connect(scoping)
stressOp3.inputs.mesh_scoping.Connect(scoping)
 
stressData1=stressOp1.outputs.fields_container.GetData()[0]
stressData2=stressOp2.outputs.fields_container.GetData()[0]
stressData3=stressOp3.outputs.fields_container.GetData()[0]
 
stressData=[]
 
for nid in curSel.Ids:
    stressData.append([nid,stressData1.GetEntityDataById(nid)[0],stressData2.GetEntityDataById(nid)[0],stressData3.GetEntityDataById(nid)[0]])
 
# Display result
mess_line='Node\tS1\tS2\tS3\n'
for sd in stressData:
    mess_line+=str(sd[0])+'\t'+str(round(sd[1],2))+'\t'+str(round(sd[2],2))+'\t'+str(round(sd[3],2))+'\n'
MessageBox.Show(mess_line)